OptiStruct
OptiStruct

2022.2

  1. Home
  2. Tutorials

    Discover OptiStruct functionality with interactive tutorials.

  3. HyperMesh Tutorials

    Tutorials using HyperMesh.

  4. Advanced Small Displacement Finite Element Analysis
  5. OS-T: 1305 Modal Frequency Response Analysis of a Flat Plate

    This tutorial demonstrates how to import an existing FE model, apply boundary conditions, and perform a modal frequency response analysis on a flat plate.

  • What's New
  • Overview
  • Tutorials
  • User Guide
  • Reference Guide
  • Example Guide
  • Verification Problems
  • Frequently Asked Questions
Index
OptiStruct

2022.2

OptiStruct
  • What's New

    View new features for OptiStruct 2022.2.

  • Overview

    OptiStruct is a proven, modern structural solver with comprehensive, accurate and scalable solutions for linear and nonlinear analyses across statics and dynamics, vibrations, acoustics, fatigue, heat transfer, and multiphysics disciplines.

  • Tutorials

    Discover OptiStruct functionality with interactive tutorials.

    • Run OptiStruct at the Command Line
    • HyperMesh Tutorials

      Tutorials using HyperMesh.

      • Run OptiStruct from HyperMesh
      • Basic Small Displacement Finite Element Analysis
      • Advanced Small Displacement Finite Element Analysis
        • OS-T: 1300 Direct Frequency Response Analysis of a Flat Plate

          This tutorial demonstrates how to import an existing FE model, apply boundary conditions, and perform a finite element analysis on a flat plate.

        • OS-T: 1305 Modal Frequency Response Analysis of a Flat Plate

          This tutorial demonstrates how to import an existing FE model, apply boundary conditions, and perform a modal frequency response analysis on a flat plate.

        • OS-T: 1310 Direct Transient Dynamic Analysis of a Bracket

          In this tutorial, an existing finite element model of a bracket is used to demonstrate how to perform direct transient dynamic analysis using OptiStruct. HyperGraph is used to post-process the deformation characteristics of the bracket under the transient dynamic loads.

        • OS-T: 1315 Modal Transient Dynamic Analysis of a Bracket

          In this tutorial, an existing finite element model of a bracket is used to demonstrate how to perform modal transient dynamic analysis using OptiStruct. HyperGraph is used to post-process the deformation characteristics of the bracket under the transient dynamic loads.

        • OS-T: 1320 Nonlinear Gap Analysis of an Airplane Wing Rib
        • OS-T: 1325 Random Response Analysis of a Flat Plate

          This tutorial demonstrates how to set up the random response analysis for the existing frequency response analysis model. The setup for frequency response analysis is that the flat plate has two loading conditions that will be subjected to a frequency-varying load excitation using the direct method.

        • OS-T: 1330 Acoustic Analysis of a Half Car Model

          The purpose of this tutorial is to evaluate the vibration characteristics of a half car model subjected to Fluid - Structure interaction. The fluid that is being referred to is air. Essentially, the noise level or the sound level is evaluated inside the car at a location near the ear of the driver which is the main response location inside the fluid.

        • OS-T: 1340 Fatigue (Stress - Life) Method
        • OS-T: 1350 Fatigue (Strain - Life) Method
        • OS-T: 1360 NLSTAT Analysis of Gasket Materials in Contact

          This tutorial demonstrates how to carry out nonlinear implicit small displacement analysis in OptiStruct involving gasket materials and contact.

        • OS-T: 1365 NLSTAT Analysis of Solid Blocks in Contact

          This tutorial demonstrates how to carry out nonlinear implicit small displacement analysis in OptiStruct, involving elasto-plastic materials, contact and continuing the nonlinear solution sequence from a preceding nonlinear loadcase.

        • OS-T: 1370 Complex Eigenvalue Analysis of a Reduced Brake System

          In this tutorial, a modal complex eigenvalue analysis is performed on a simplified brake system to determine whether the friction effects can cause any squeal noise (unstable modes).

        • OS-T: 1371 Brake Squeal Analysis of Brake Assembly

          In this tutorial you will perform a brake squeal analysis on a brake assembly. Disc brakes are operated by applying a clamping load using a set of brake pads on the disc. The friction generated between the pads and the disc causes deceleration, and can potentially induce a dynamic instability of the system. This phenomena is known as brake squeal.

        • OS-T: 1372 Rotor Dynamics of a Hollow Cylindrical Rotor

          In this tutorial you will perform Rotor Dynamics analysis on a hollow cylindrical rotor.

        • OS-T: 1375 Response Spectrum Analysis of a Structure

          This tutorial demonstrates how to perform a Response Spectrum Analysis on a structure.

        • OS-T: 1380 Computation of Equivalent Radiated Power

          Computation of the equivalent radiated power (ERP) is a simplified method to gain information about maximum dynamic radiation of panels for excitations in frequency response analysis. This tutorial demonstrates how to set up the computation request of ERP on an existing frequency response analysis.

        • OS-T: 1385 Heat Transfer Analysis on Piston Rings using Thermal Contact

          Piston rings fit on the outer surface of a piston in an engine and they transfer heat from the piston to the cylinder wall.

        • OS-T: 1390 Pretensioned Bolt Analysis of an IC Engine Cylinder Head, Gasket and Engine Block System

          This tutorial outlines the procedure to perform both 1D and 3D pretensioned bolt analysis on a section of an IC Engine. The pretensioned analysis is conducted to measure the response of a system consisting of the cylinder head, gasket and engine block connected by four head bolts subjected to a pretension force of 4500 N each.

        • OS-T: 1392 Node-to-Surface versus Surface-to-Surface Contact

          This tutorial demonstrates how to set up contact between two parts and the impact of using choosing node-to-surface (N2S) versus surface-to-surface (S2S). In addition, this tutorial covers how to review the internally created CGAPG elements in case of N2S, and the nodes in contact in case of S2S.

        • OS-T: 1393 Basics of Contact Properties and Debugging

          This tutorial demonstrates the effect of using contact stabilization, clearance, and adjust.

        • OS-T: 1394 Axi-Symmetric Ball Joint

          This tutorial demonstrates how to carry nonlinear analysis for Axi-symmetric ball joint for pull load of 10,000N using OptiStruct.

        • OS-T: 1395 Acoustic Analysis of Speaker Using RADSND

          This tutorial demonstrates how to perform acoustic analysis of 2.1 speakers using the RADSND Method.

      • Large Displacement Finite Element Analysis
      • Fluid-Structure Interaction Analysis
      • Multibody Dynamics Analysis
      • Topology Optimization
      • Topography Optimization
      • Combination Optimization
      • Size Optimization
      • Shape Optimization
      • Fatigue Analysis
      • Nonlinear Explicit Analysis

        This section presents nonlinear explicit analysis examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.

      • Aeroelastic Analysis

      • Third Party Interface

    • HyperWorks Tutorials

      Tutorials using HyperWorks.

    • SimLab Tutorials

      Video tutorials using SimLab.

  • User Guide

    This manual provides detailed information regarding the features, functionality, and simulation methods available in OptiStruct.

  • Reference Guide

    This manual provides a detailed list and usage information regarding input entries, output entries, and parameters available in OptiStruct.

  • Example Guide

    The OptiStruct Example Guide is a collection of solved examples for various solution sequences and optimization types and provides you with examples of the real-world applications and capabilities of OptiStruct.

  • Verification Problems

    This manual presents solved verification models including NAFEMS problems.

  • Frequently Asked Questions

    This section provides quick responses to typical and frequently asked questions regarding OptiStruct.

View All Altair Simulation Help

OptiStruct
OptiStruct

2022.2

  1. Home
  2. Tutorials

    Discover OptiStruct functionality with interactive tutorials.

  3. HyperMesh Tutorials

    Tutorials using HyperMesh.

  4. Advanced Small Displacement Finite Element Analysis
  5. OS-T: 1305 Modal Frequency Response Analysis of a Flat Plate

    This tutorial demonstrates how to import an existing FE model, apply boundary conditions, and perform a modal frequency response analysis on a flat plate.

  • What's New
  • Overview
  • Tutorials
  • User Guide
  • Reference Guide
  • Example Guide
  • Verification Problems
  • Frequently Asked Questions
Index

OS-T: 1305 Modal Frequency Response Analysis of a Flat Plate

This tutorial demonstrates how to import an existing FE model, apply boundary conditions, and perform a modal frequency response analysis on a flat plate.

Before you begin, copy the file(s) used in this tutorial to your working directory.
  • modal_response_flat_plate_input.fem

The flat plate is subjected to a frequency varying unit load excitation using the modal method. Post-processing tools will be used in HyperView and HyperGraph to visualize deformations, mode shape response, and frequency-phase output characteristics.

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. Select OptiStruct and click OK.
    This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Import the Model

  1. Click File > Import > Solver Deck.
    An Import tab is added to your tab menu.
  2. For the File type, select OptiStruct.
  3. Select the Files icon files_panel.
    A Select OptiStruct file browser opens.
  4. Select the modal_response_flat_plate_input.fem file you saved to your working directory.
  5. Click Open.
  6. Click Import, then click Close to close the Import tab.

Set Up the Model

Apply Loads and Boundary Conditions

In the following steps, the model is constrained at one edge. A unit vertical load is applied acting upwards in the positive z-direction at a point on a free edge corner of the plate. First, the two load collectors (spcs and unit-load) are created.
  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter spcs.
  3. Click Color and select a color from the color palette.
  4. For Card Image, set to None.
    A new load collector, spcs is created.
  5. In the Model Browser, right-click and select Create > Load Collector.
  6. For Name, enter unit-load.
  7. Click Color and select a color from the color palette.
    A new load collector, unit-load is created.
  8. Click the Display Numbers icon infoNumbers-24 to open the Numbers panel.
  9. Click nodes > displayed.
  10. Check the box next to display.
  11. Select the green on button.
    All of the node numbers on the flat plate should now be displayed.

Create Constraints

  1. In the Model Browser, right-click the load collector spcs and select Make Current.

    rd2000_spc_load_collector
    Figure 1.
  2. Click BCs > Create > Constraints to open the Constraints panel.
  3. Click the entity selection switch and select nodes from the pop-up menu.
  4. Click nodes and select nodes 5, 29, 30, 31 and 32 (see Figure 2).

    os1100_pic1
    Figure 2. Illustration of Nodes to Select for Applying Single Point Constraints
  5. Constrain dof1, dof2, dof3, dof4, and dof5.
    • DOFs with a check will be constrained while DOFs without a check will be free.
    • DOFs 1, 2, and 3 are x, y, and z translation degrees of freedom.
    • DOFs 4, 5, and 6 are x, y, and z rotational degrees of freedom.
  6. Click create.
    The selected nodes will be free to rotate about the z-axis since dof6 was not checked.
  7. Click return to go back to the main menu.

Create a Unit Load at a Point on the Flat Plate

  1. In the Model Browser, right-click on the load collector unit-load and select Make Current.
  2. Click BCs > Create > Constraints to open the Constraints menu.
  3. Select node number 19 on the plate by clicking on it (Figure 3).

    os1100_pic2
    Figure 3. Node Selected for Creating Unit Vertical Load
  4. Uncheck all the dof's except dof3 and click the = to the right of dof3 and enter a value of 1.
  5. Click load types= and verify that DAREA is selected from the extended entity selection menu.
  6. Click create, and then click return.
    The unit load is applied to the selected node.

Create a Frequency Range Table

  1. In the Model Browser, right-click and select Create > Curve.
    A new window opens.
  2. For Name, enter tabled1.
  3. In the table, enter x(1) = 0.0, y(1) = 1.0, x(2) = 1000.0, y(2) = 1.0.
  4. Close the Curve Editor window.
  5. From Curves, select tabled1.
  6. For Type, select TABLED1 from the drop-down menu.
    This provides a frequency range of 0.0 to 1000.0 with a constant 1.0 over this range.

Create a Frequency Dependent Dynamic Load

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
  2. For Name, enter rload2.
  3. For Config type, select Dynamic Load – Frequency Dependent from the drop-down list.
  4. For Type, and select RLOAD2 from the drop-down list.
  5. For Excited, click Unspecified > Loadcol.
  6. In the Select Loadcol dialog, select unit-load from the list of load collectors and click OK to complete the selection.
  7. For TB, select the tabled1 curve.
    The type of excitation can be an applied load (force or moment), an enforced displacement, velocity or acceleration. The field Type in the RLOAD2 load step input defines the type of load. The type is set to applied load by default.

Create a Set of Frequencies

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter freq1.
  3. Click Color and select a color from the color palette.
  4. For Card Image, select FREQi from the drop-down menu.
  5. Check the FREQ1 option and enter 1 in the NUMBER_OF_FREQ1 field.
  6. Update the following fields in the pop-out window.
    1. For F1, enter 20.0.
    2. For DF, enter 20.0.
    3. For NDF, enter 49.
  7. Click Close.
    This provides a set of frequencies beginning with 20.0, incremented by 20.0 and 49 frequencies increments.

Create the Modal Method for Eigenvalue Analysis

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
  2. For Name, enter eigrl.
  3. Click Color and select a color from the color palette.
  4. For Config type, select Real Eigen Value Extraction.
  5. For Type, select EIGRL.
  6. Click V1 and enter a value 0.0, then click V2 and enter a value of 1000.0.
    This specifies a range of frequency between 0 Hz and 1000 Hz for eigenvalue extraction using the Lanczos method.

Create a Load Step

  1. In the Model Browser, right-click and select Create > Load Step.
    A default load step template is now displayed in the Entity Editor below the Model Browser.
  2. For Name, enter subcase1.
  3. For Analysis type, select Freq.resp (modal) from the drop-down menu.
  4. For METHOD(STRUCT), select Unspecified > Load step inputs.
  5. From the Select Load Step Inputs dialog, select eigrl.
  6. For SPC, select Unspecified > Loadcol.
  7. From the Select Loadcol dialog, select spcs.
  8. For DLOAD, select rload2 from the Select Load Step Inputs pop-out window.
  9. For FREQ, click Unspecified > Loadcol
  10. From the Select Loadcol dialog, select freq1.
    An OptiStruct subcase is created which references the constraints in the load collector spc, the unit load in the load step input rload2 with a set of frequencies defined in load collector freq1 and modal method defined in the load step input eigrl.

Create a Set of Nodes

  1. In the Model Browser, right-click and select Create > Set.
  2. For Name, enter SETA.
  3. For Card Image, select None.
  4. Leave the Set Type switch set to non-ordered type.
  5. For Entity IDs, select Nodes from the selection switch.
  6. Click Nodes and select nodes with IDs 15, 17 and 19.
  7. Click proceed.

Create a Set of Outputs and Mass Factors

  1. Click Setup > Create > Control Cards to open the Control Cards panel.
  2. Select GLOBAL_OUTPUT_REQUEST and check the box next to DISPLACEMENT.
  3. Click the field box FORM(1) and select PHASE from the pop-up menu.
  4. Click the field box OPTION(1) and select SID from the pop-up menu.
    A new field appears in yellow.
  5. Double-click the yellow SID box and select SETA from the pop-up selection on the bottom left corner.
    A value of 1 now appears below the SID field box. This sets the output for only the nodes in set 1.
  6. Click return to exit the GLOBAL_OUTPUT_REQUEST menu.
  7. Click next and select the PARAM subpanel.
  8. Scroll down the list using the arrow in the left corner and check the box next to COUPMASS.
    A new PARAM card appears in the work area screen.
  9. Below COUPM_V1 click NO and select YES from the pop-up menu selection.
    Selecting YES uses the coupled mass matrix approach for eigenvalue analysis.
  10. Check the box next to G.
    A new window appears in the work area screen.
  11. Click below G_V1, and enter a value of 0.06 into the field box.
    This value specifies a uniform structural damping coefficient and is obtained by multiplying the critical damping [ C / C 0 MathType@MTEF@5@5@+= feaagKart1ev2aaatCvAUfeBSjuyZL2yd9gzLbvyNv2CaerbuLwBLn hiov2DGi1BTfMBaeXatLxBI9gBaerbd9wDYLwzYbItLDharqqtubsr 4rNCHbGeaGqiVu0Je9sqqrpepC0xbbL8F4rqqrFfpeea0xe9Lq=Jc9 vqaqpepm0xbba9pwe9Q8fs0=yqaqpepae9pg0FirpepeKkFr0xfr=x fr=xb9adbaqaaeGaciGaaiaabeqaamaabaabaaGcbaGaam4qaiaac+ cacaWGdbWaaSbaaSqaaiaaicdaaeqaaaaa@391F@ ] ratio by 2.0.
  12. Scroll down using the arrow to the left corner and check the box next to WTMASS.
    A new window appears in the work area screen.
  13. Click below WTM_V1, and enter a value of 0.00259 into the field box.
    Three PARAM statements now appear in the pop-up menu on the work screen.
  14. Click return to exit the PARAM menu.
  15. Select the OUTPUT card.
    A new window appears in the work area.
  16. In the number_of_outputs field, enter 3.
  17. Set the first KEYWORD to HGFREQ.
    Using HGFREQ results in a frequency output presentation for HyperGraph.
  18. Set the second KEYWORD to OPTI.
  19. Set the third KEYWORD to H3D.
  20. Double-click on the box beneath FREQ and select ALL from the pop-up selection for all keywords.
    Selecting ALL will output all optimization iterations.
  21. Click return to exit OUTPUT.
  22. Click return to exit the Control Cards menu.

Submit the Job

  1. From the Analysis page, click the OptiStruct panel.

    OS_1000_13_17
    Figure 4. Accessing the OptiStruct Panel
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter flat_plate_modal_response for filename.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct to launch the OptiStruct job.
If the job is successful, new results files should be in the directory where the flat_plate_modal_response.fem was written. The flat_plate_modal_response.out file is a good place to look for error messages that could help debug the input deck if any errors are present.
The default files written to the directory are:
flat_plate_modal_response.html
HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
flat_plate_modal_response.out
OptiStruct output file containing specific information on the file setup, the setup of your optimization problem, estimates for the amount of RAM and disk space required for the run, information for each of the optimization iterations, and compute time information. Review this file for warnings and errors.
flat_plate_modal_response.h3d
HyperView binary results file.
flat_plate_modal_response.res
HyperMesh binary results file.
flat_plate_modal_response.stat
Summary, providing CPU information for each step during analysis process.

Review the Results

This step describes how to view displacement results (.mvw file) in HyperGraph and also how to understand the displacement output (.disp file) from this run. The HyperView results file (.h3d) contains only the displacement results for the three nodes specified in the node set output.
  1. From the OptiStruct panel, click HyperView.
    HyperView is launched and the results are loaded. A message window appears to inform of the successful model and result files loading into HyperView.
  2. Click Close to close the message window, if one appears.
  3. In the HyperView window, click File > Open > Session.
    An Open Session File window opens.
  4. Select the directory where the job was run and select file flat_plate_modal_response_freq.mvw.
  5. Click Open.
    A discard warning appears.
  6. Click Yes.
    Two graphs per page and a total of three pages are displayed in HyperGraph. The graph title shows Subcase 1 (subcase 1) - Displacement of grid 15 on page 1.
  7. Click the Axis toolbar icon annotateAxes-24. Select Logarithmic option and use the parameters shown below to make logarithmic plots of the results.

    rad_logarithmic
    Figure 5.
    There are two sets of results on this page. The top graph shows Phase Angle verses Frequency (log). The bottom graph shows Magnitude verses Frequency (log) (see figure) for Displacement of grid 15.

    rd2010_results15
    Figure 6. Frequency response of node 15
  8. Directly underneath the blue graph border, click the Next Page icon pageNext-24.
    Page 2 displays, which shows Subcase 1 (subcase1) - Displacement of grid 17.

    rd2010_results17
    Figure 7. Frequency Response of Node 17
  9. Click the Next Page icon pageNext-24 again to display page 3 containing Subcase 1 (subcase1) - Displacement of grid 19.

    rd2010_results19
    Figure 8. Frequency Response of Node 19
    This concludes the HyperGraph results processing.
  10. Open the displacement file (.disp) using a text editor.
    The first field on the second line shows the iteration number, the second field shows number of data points, and the third field shows iteration frequency.

    Line 3, first field shows node number, then x, y and z displacement magnitudes and x, y and z rotation magnitudes.

    Line 4, first field shows node number, then x, y and z displacement phase angles and x, y and z rotation phase angles.

© 2022 Altair Engineering, Inc. All Rights Reserved.

Intellectual Property Rights Notice | Technical Support | Cookie Consent